Learning Forum

[Naji Al-Abed]

Hello, From modal analysis on Ansys I got all the 6 modes with their natural frequencies and their mode shapes to see how the beam acts. I just wanted to know how can I plot the modal damping ratio at each mode number against the system's natural frequency?I tried extracting it using the piezoandmems extension, where there there is a solutio otion for the damping modal coefficients but I keep getting this error. I tried this step as recommended by Surya: "Go to Analysis Settigs > Output Controls and change all the options to Yes" but nothing worked.

 

[Dave Looman]

I made a model with a spring-damper so there would be some mode-dependent damping.  Then I ran the modal with a damped solver (Reduced Damped.)  After the solution I highlighted Solution (A6) and got the table below.

[Naji Al-Abed]

Dear Dave,
Thank you for your response, I see the results but I don't see the methods applied. May I please meet with you or anyone of your colleagues over a call to discuss this query. It is very urgent.
Kind Regards,
Naji

[Dave Looman]

Do you have access to support through the normal channel, submitting support request on the customer portal?

[Naji Al-Abed]

I am getting asked of a customer number but I have never been assigned one. I just need someone to discuss this with me over a  teams call, feel it will be much more benefical as compared to me posting on the forum and waiting 3-4 days.
Kind Regards,
Naji

[Dave Looman]

Forum support doesn't include having a Teams Meeting.  If you can explain in detail what you are asking I'll attempt to help you expeditiously.

[Naji Al-Abed]

Its the question I was initially asking, the reply you posted just includes the results, there was no method mentioned on what controls or forces to input to obtain the damping ratio.

[Dave Looman]

You should have some sort of material dependent damping or a damped spring.  Of course that information is hard to find.

[Naji Al-Abed]

Sorry, I appreciate your response but is there anyone else that can help me?

[Ashish Kumar]

Hi,

Technical Support for Ansys products is provided either by Ansys directly or by one of our certified Ansys Support Providers. Please check with the Ansys support coordinator (ASC) at your company to determine who provides support for your company, or visit the Contacts and Locations page.

If your support is provided by Ansys directly, Technical Support can be accessed quickly and efficiently from the Ansys Customer Portal. The direct URL is: https://customer.ansys.com.

If you are an academic user including professors, researchers and students, support is handled through our Ansys Learning Forum found at: ansys.com/forum.

When inquiring by phone or email, please have your customer number ready in advance. Find out how to retrieve your customer number here.

One of the many useful features of the Customer Portal is the Knowledge Resources Search, which can be found on the home page of the Customer Portal.

For more details check this page: Contacting Technical Support | Ansys IT Solutions

Regards,

Ashish Kumar

[Bill Bulat]

 

Hi Naji. I suggest you please use a Coupled Field Modal analysis system (rather than the Piezo & MEMS ACT) to do your modeling. Piezoelectric analyses are now natively exposed in Coupled Field analysis systems. The Piezo and MEMS ACT is no longer supported and the last version may not be fully functional in later versions of ANSYS. Also, we now have a library of piezoelectric material properties in Engineering Data that you can use in Coupled Field analysis systems.

I created a small piezoelectric test case using a Coupled Field Modal analysis system to help explain one way to get modal damping ratios from a modal analysis of a piezoelectric device. I cannot share it with you on the Forum - we're not allowed to do that. But I can capture images from the project that should help you get started.

By default, our modal analyses use an undamped eigensolver that makes no effort to include damping in the calculation of natual frequencies and mode shapes. The default undamped solver will not provide any information allowing you to deduce damping ratio associated with calculated natural frequencies.

So, as Dave said earlier in this thread, to get a damping ratio from a modal analysis, you must do two things:

Use the damped eigensolver (image below). Either the "full damped" or "unsymmetric" option will do, but in your case full damped might be better - in addition to giving you the stability of the mode, it will explicitly report the damping ratio (your objective) in a table.

The other thing you need to do is define some source of damping. In my test case, I have no structural damping, only an isotropic electric loss tangent that I added to our predefined Barium Titanate properties in Engineering Data:

I model a fixed-fixed beam, atop which resides a piezoelectric transducer with VOLT coupled (an open electrode/terminal) on the top surface and VOLT=0 (grounded) on the bottom surface:

With loss tangent = 0.002, the calculated damping ratio of the first mode is 1.836e-6:

With loss tangent = 0.2, the calculated modal damping ratio is 1.798e-4:

 

Also, many people who analyze piezoelectric devices want to include the effect of passive circuit elements connected across the terminals of the transducer (an electrical load of some kind). As this is not yet natively exposed, this requires a command object that creates CIRCU94 elements:

I hope this helps.

Kind regards,

Bill

 

 

 

 

 

 

[Bill Bulat]

I forget to mention, it appears you are using a post processing tool that is intended to extract damping ratio associated with squeeze film elements (which are usually used to model the gas - air - occupying a thin gap between a MEMS device, e.g., micro mirror, and the substrate beneath it):

 

Your assembly does not appear to be a MEMS device (with dimensions on the micron-to-single millimeter scale), nor does it appear to have squeeze film elements in it. In short, the post processing object you appear to be using almost certainly does not pertain to your model.

Best,

Bill

[Naji Al-Abed]

Dear Bill,
Thank you very much for your response. I am understanding it better now but I can't place a damping factor for aluminum in the engineering data as in I am unable to type the value in. What would you suggest?

Kind Regards,
Naji

[Naji Al-Abed]

 

Dear Bill,

Sorry for the many questions but I ahve tried using Coupled field harmonic analysis to analyze the voltage frequency response curve but I am only getting a horizontal straight line. Basically, this system consists of 2 piezoelectric patches on either side of the beam, and  a bluff body. I have applied 2 forces( where these forces are drag forces experienced when in the wind tunnnel), one on the bluff body and one on the beam. I have also placed a voltage ground on one patch(red) and another voltage (100V) on the other patch. However, I can’t get a proper voltage frequency graph. I have tried looking for videos relating this tab but was unable to find any. Thank you.

Kind Regards,
Naji

 

[peteroznewman]

Bill, thank you for the steps needed to build a Piezoeletric model. I tried it out in ANSYS 2023 R2 and it is easy to build the model.

I added on a Coupled Harmonic analysis and got a Voltage Frequency Response. Naji, I don't see a Voltage Coupling item in your model.

[Naji Al-Abed]

Dear Peteroznewman,
Where should I add the voltage coupling in my model if I want to measure the voltage response across the piezoelectric patches(highlighted in red) considering I placed a ground voltage across one of the patches?
Kind Regards,
Naji

[peteroznewman]

Dear Naji,

In my model, the Voltage Ground is on the face of the piezo patch facing the metal plate, the Voltage Coupling is on the opposite face of the patch following the example Bill showed in his model.

Regards,
Peter

[Naji Al-Abed]

Dear Peteroznewman and Bill,
Would you happe to know why I am a getting a graph with such low voltage amplitudes? Thank you.
Kind Regards,
Naji